Totempole pfc control loop

thaamike · July 16, 2026, 10:42am

Hi all,

I’m trying to make a totempole pfc for the first time. I want to see if i can make it work in qspice.
I want to use the dll block to simulate a digital control loop.
But i have issues with it.

My feedforward alone shows wave current that i think is not correct. See below with anly the feedforward.

This is the code i have un my mcu dll file:

// Automatically generated C++ file on Wed Jul 15 11:30:01 2026
//
// To build with Digital Mars C++ Compiler:
//
// dmc -mn -WD -o mcu_calc_2.cpp kernel32.lib

union uData
{
bool b;
char c;
unsigned char uc;
short s;
unsigned short us;
int i;
unsigned int ui;
float f;
double d;
long long int i64;
unsigned long long int ui64;
char *str;
unsigned char *bytes;
};

// int DllMain() must exist and return 1 for a process to load the .DLL
// See DllMain entry point (Process.h) - Win32 apps | Microsoft Learn for more information.
int __stdcall DllMain(void *module, unsigned int reason, void *reserved) { return 1; }

// #undef pin names lest they collide with names in any header file(s) you might include.
#undef Vac_in
#undef Iac_in
#undef Vout
#undef PWM_H
#undef PWM_L
#undef SYNC_H
#undef SYNC_L
#undef clk
#undef tmp
#undef tmp2
#undef tmp3

extern “C” __declspec(dllexport) void mcu_calc_2(void **opaque, double t, union uData *data)
{
// Inputs
double Vac_in = data[0].d;
double Iac_in = data[1].d; // Dit is je gemeten stroom
double Vout = data[2].d;
bool clk = data[3].b;

// Outputs
double &PWM_H  = data[4].d;
double &PWM_L  = data[5].d;
double &SYNC_H = data[6].d;
double &SYNC_L = data[7].d;
double &tmp    = data[8].d;
double &tmp2   = data[9].d;
double &tmp3   = data[10].d;


static double integrator = 0.0;
static double vout_filt  = 400.0;
static bool   prev_clk   = false;


double Kp = 0.9; // Proportionele versterking
double Ki = 0.01;  // Integrale versterking


if (clk && !prev_clk)
{
    // 1. Schaling
    double vac_real = (Vac_in - 1.65) / (4300.0 / 1004300.0);
    double vout_real = Vout / (4300.0 / 514300.0);
    vout_filt = (0.999 * vout_filt) + (0.001 * vout_real);

    double iac_real = (Iac_in - 1.65) / 10;
    double abs_iin = (iac_real < 0) ? -iac_real : iac_real;
    double i_ref = vac_real * 0.00001; // Schaalfactor afhankelijk van je load
    double abs_iref = (i_ref < 0) ? -i_ref : i_ref;

    // 2. Referentie genereren (De gewenste stroomvorm)
    // De referentie is in fase met de Vac (abs_vin)
    double abs_vin = (vac_real < 0) ? -vac_real : vac_real;

    // 3. PI-berekening
    //double error = abs_iref - abs_iin ;
    double error = abs_iin  - abs_iref ;

    integrator += error * Ki;

    // Anti-windup (beperk de integrator)
    if (integrator > 0.2) integrator = 0.2;
    if (integrator < -0.2) integrator = -0.2;

    double pi_output = (error * Kp) + integrator;

    // 4. Feedforward + PI output
    double d_ff = 1.0 - (abs_vin / (vout_filt + 1.0));

    tmp = abs_iref;
    tmp2 = abs_iin;
    tmp3 = pi_output;



    double d_total = d_ff ;//+ pi_output;

    // 5. Clamping
    if (d_total > 0.99) d_total = 0.99;
    if (d_total < 0.01) d_total = 0.01;

    // 6. PWM & SYNC aansturing
    if (vac_real > 0.05) {
        SYNC_H = 3.3; SYNC_L = 0.0;
        PWM_H = d_total;
        PWM_L = 1.0 - d_total;
    } else if (vac_real < -0.05) {
        SYNC_H = 0.0; SYNC_L = 3.3;
        PWM_H= 1.0 - d_total; 
        PWM_L = d_total; 
    } else {
        SYNC_H = 0.0; SYNC_L = 0.0;
        PWM_H = 0.0;
        PWM_L = 0.0;
        //integrator=0;
    }
}
prev_clk = clk;

}

Anyone an idea why this is happening ??

macsky · July 16, 2026, 10:58am

Could you upload the .qsch and C++ code, it would be helpful for anyone who is going to do a detailed review.

thaamike · July 16, 2026, 11:07am

Here it is:

pfc_ccm.qsch (52.2 KB)
mcu_calc_2.cpp (3.6 KB)

thaamike · July 16, 2026, 11:25am

I delay my clk pulse block so it matches with the middel of the triagle. the waveform is a lot better. But i still do not understand the phase delay. That is so big.

This is the waveform with just the feedforward.

thaamike · July 16, 2026, 11:30am

maybe i dont have proper center aligned pwm …?

thaamike · July 16, 2026, 1:44pm

ofcourse it has a delay.. it’s an inductor.
But when i try using a simple pi control, i get massive overshoot on the second part of the sinewave

.

physicboy · July 16, 2026, 3:10pm

Are you Dutch? The comment looks familiar to me as an Indonesian…though many of it I don’t understand.

Anyway, your code should be kept inside data struct. When you generate the template you need to enable this option.

The purpose is to ensure the data integrity when the Spice do abandon the “hypothetical timestep”.

I have many examples in my Github on digital control converter.
The simpler one is : QSPICE/PWM_example_SRbuck at main · physicboy/QSPICE · GitHub

There is also 3P4W grid tie inverter.

Just a sidenote,

I use a very fast (though complex) digital PWM generation, which make my code run very fast, but harder to understand for beginner.
Most of my PWM is based on center aligned, including one used in these SRbuck and 3P4W inverter

Arief,

thaamike · July 16, 2026, 3:27pm

yes i’m dutch.

I made many power conveters in the past including DAB etc(from few 100W up to 50kW. But mainly the power stage, topology and magnetics part. Digital control i have limited experience with but i want to learn this more.

That said, i want to use this to set up digital control. BUt want to have it working first ofcourse.

Would you mind helping me change my code to make it better suited ?

ps. My control does not work well because i invert the duty in the output code. This means that the second part of the sinewave, the control operates the wrong direction. I think i should take the direction outside the block for now.

physicboy · July 16, 2026, 4:24pm

The easiest thing for you to try is to add

if(*ForKeeps==0)return;

at the very first line of the eval_func()

This one will ensure that the rest of the code won’t get called while the sim is using “hypothetical timestep”.

If the logic on the rest of the code is correct, that trick should do the work.

KSKelvin · July 16, 2026, 4:33pm

He needs an external clock, and the correct way is to include Trunc() for hypothetical calls.
His schematic has ¥-Device, which by default includes TTOL (equivalent as Trunc()). So, I guess skipping hypothetical calls may mess up the whole thing…

Here is code to demonstrate sampling V(in) at every rising edge of V(clk) by including Trunc() to reduce the timestep to TTOL at the rising edge.
In this example, I added timectrl=none for V2. The purpose is to remove the timestep control algorithm in V2 so that I can clearly demonstrate the use of Trunc() in this C code only modify rising edge, and not at the falling edge. If timectrl=none is removed from V2, you will see the timestep also reduce at the clock falling edge, as V2 has its own timestep control to help reduce the timestep at transitions.
Cblock.qsch (2.5 KB)
cblock.cpp (5.0 KB)

thaamike · July 17, 2026, 3:31pm

thank you both for helping me out. I used the code from Kelvin and put it in mine. I do see some behavior i did not expect. See below for the waveform. I am sampling at 100kHz but there is a change in value during the cycle. I would expect a more block wave if you will. Any idea how this happens?
mcu_calc_2.cpp (7.6 KB)

KSKelvin · July 17, 2026, 5:58pm

I think your schematic requires two .cpp files, and you haven’t uploaded the other one. Please consider uploading all the necessary files again.

thaamike · July 17, 2026, 7:25pm

pll_srf.cpp (4.0 KB)
here is the other one. I dont use any output yet. Could this be the reason for the change in values between clock cycles ?

thaamike · July 17, 2026, 10:16pm

I cleaned up a little and took out the polarity change in the code and used logic blocks. Getting the same feedforward effect so that seems the same. But still not current controlled and get strange behavior i dont understand .
pfc_ccm.qsch (67.1 KB)
mcu_calc_2.cpp (7.8 KB)

Darrell_Hambley · July 18, 2026, 5:57pm

Thaamike, It would help us a lot if you could simply write down the control equations that your are trying to implement for the pulse widths in algebraic form. (such as: Duty = K*sinVac . . . etc etc) first instead of the code to implement the control equations. It looks like people are suggesting canned code with no understanding of what’s in there.

thaamike · July 18, 2026, 7:53pm

Well i want to keep it simple to start with and use only a closed current loop.
At the moment i only have feedfoward that is a rectified sinusodial shape. I take the abs value of both voltages and currents.

My plan is using a slow PI control first. Meaning i take the error between measured and ref current and put that is my pi. output is between 0.1 and 0.99 and is compared with triagle waveform that go’s from 0 to 1.

I make the current ref by multiplying the rectified ac voltage.

KSKelvin · July 19, 2026, 10:59am

@thaamike Did you have a working analog model before you implemented the C++ model?
I cannot run your code because you included a subcircuit that needs MyLibrary.lib, and you didn’t upload that file.

A totem-pole PFC is a topic I am not familiar with. For a new topic, my approach is to build an analog model and verify everything step by step after learning how things work fundamentally. Once the analog model works, you can move forward to C++ code for the controller.

I didn’t close the voltage loop or implement discrete sampling in this code, as by the time I reached this point, I had already spent a few hours on it. I hope this can be a starting point for anyone who needs to work on a totem-pole PFC in QSpice.
I recommend that you use ideal devices for the initial implementation. After you get things working, you can step by step replace parts of your circuit with semiconductor models.

PFC-totem-pole (analog version).qsch (27.9 KB)

PFC-totem-pole (C++ version).qsch (14.7 KB)
totempole_pfc.cpp (6.5 KB)

thaamike · July 19, 2026, 12:58pm

HI,

Thank you for the time you put into this. This will for sure help me . I already spend days in this trying to figure out what i’m doing wrong. I’m to green in this simulation part.
Somehow i always have difficulties with simulations…

I tried a simple pfc stage boost and get some osscilation near the zero crossing for example.

But that for another time i think. I will use you exmaple as a start form now on. Thank you very much.

thaamike · July 19, 2026, 1:07pm

Could you explain to me why use used a gain of 1e6?

KSKelvin · July 19, 2026, 1:39pm

Here is the Bode plot of an integrator with 1e6 gain, where its crossover frequency is at ~160kHz, which is roughly the switching frequency in this example. You might wonder why this number is so large, but an integrator gain between 1e4 and 1e6 is actually quite common for an SMPS.

In my experience, the easiest way to tune a PI controller is to first apply the I gain with the P gain set to 0. Increase the I gain by orders of 10 to check the response. Once you have a good enough I gain, move on to applying the P gain. The P gain generally starts from a very small number (e.g., 0.01) and is increased to see the response. Of course, the best approach is to obtain the open-loop response and design the controller, but it is also common to tune it blindly, as that is the beauty of a PI controller.

Most importantly, I actually don’t know how to measure the open-loop response of the current loop in this totem-pole PFC. If anyone knows how to do that, sharing it would be very helpful.